[brenlee42]

I'm almost capable of manually programming, I just need a better understanding
of G02 & G03.

I know what they mean, I just have no idea how to actually do the math
to figure it out.

I usually use Mastercam to program, but it's pricey and getting old. Any
help would be much appreciated.

[Geof]

Give a sketch for a piece you want to program and I will try to give a clear example.

[txcncman]

I'm almost capable of manually programming, I just need a better understanding
of G02 & G03.

I know what they mean, I just have no idea how to actually do the math
to figure it out.

I usually use Mastercam to program, but it's pricey and getting old. Any
help would be much appreciated.

Have you read the Haas manual on G02 and G03 commands? Do you understand the terms "incremental distance", "start point of arc", and "center point of arc"?

[brenlee42]

Geof:
The ID is 1.251
the OD is 1.875
Got .002 to play with on the ID.
Thank you for the help!

[brenlee42]

I have. I understand that G02 is CW and G03 is CCW. And I do understand centerpoint of arc. The rest, when it comes to hand writing. I'm clueless.

[Geof]

Geof:
The ID is 1.251
the OD is 1.875
Got .002 to play with on the ID.
Thank you for the help!

I notice in your thread about tool compensation your are machining a hub (or something).

You do not mention the size of the starting material so I will write a program starting with 2" OD material. You also do not mention how deep you want to go so again I will choose a distance of 1.75". I will also choose to use a 1/2" cutter. Also I will choose to place my work zero at the center of the hole because it makes the programming easier.

This should work. If you do not have a Haas manual go to the Haas website and you can download a copy. It will help you understand things.


%
O00000 (BUSHING)
N1 G00 G20 G40 G49 G80 G90 G98
N2 G53 G00 Z0.
N3 G10 L12 G90 P1 R0.5 (THIS ENTERS THE TOOL DIA. INTO THE OFFSET TABLE)
N5 (-------)
N6 T1 M06 (1/2 MILL)
N7 G43 H01
N8 S3000 M03
(LINES N9 TO N13 INTERPOLATE THE OD)
N9 G54 G00 X0. Y1.6 Z1. (THE G54 WORK ZERO IS AT THE CENTER OF THE PART)
(LINE N9 POSITIONS THE TOOL AT THE START, CLEAR OF THE OD AND ABOVE THE PART)
N10 G41 D01 X0. Y0.9375 Z0.01
(LINE N10 STARTS TOOL COMPENSATION AND MOVES THE TOOL JUST ABOVE THE PART)
N11 G91 G02 I0. J-0.9375 Z-0.1 F20. L15
(LINE N11 HELICALLY INTERPOLATES DOWN 1.5 INCHES USING INCREMENTAL)
N12 G90 G02 I0. J-0.9375 Z-1.5 L2
(LINE N12 CLEANS UP THE RAMP AT THE END OF THE HELICAL INTERPOLATION)
N13 G01 X0.2
N14 Z0.1
N15 G40 X0. Y0.
(N13 TO 15 MOVE THE TOOL AWAY FROM THE PART, LIFTS IT ABOVE THE PART AND)
(CANCEL TOOL COMPENSATION AS THE TOOL MOVES TO THE CENTER OF THE PART)
(LINES N16 TO N23 INTERPOLATE THE ID TAKING)
N16 G41 D01 X0. Y0.5 Z0.01
(LINE N16 STARTS TOOL COMP AND POSITIONS THE TOOL FOR A ROUGHING CUT)
N17 G91 G03 I0. J-0.5 Z-0.1 F20. L15
(LINE N17 HELICALLY INTERPOLATES DOWN 1.5 INCHES)
N18 G90 G03 I0. J-0.5 Z-1.5 L2 (CLEANS UP BOTTOM)
N19 G40 G00 X0. Y0. Z0.1 (CANCEL TOOL COMP MOVE TO TOP)
N20 G41 D01 X0. Y0.6255 Z0.01 (SET TOOL COMP AND FINAL SIZE)
N21 G91 G03 I0. J-0.6255 Z-0.1 F20. L5
N22 G90 G03 I0. J-0.6255 Z-1.5 L2
N23 G40 G00 X0. Y0. Z1. (CANCEL TOOL COMP AND MOVE CLEAR)
(THE SEQUENCE FROM N16 TO N23 COULD BE REPEATED FOR A SPRING)
(PASS TO CORRECT FOR TOOL DEFLECTION)
N24 G53 G00 Z0. (MOVE THE TOOL UP TO THE TOOL CHANGE POSITION OUT OF THE WAY)
N25 M30 (END PROGRAM)
%

[JohnJW]

I'm almost capable of manually programming, I just need a better understanding
of G02 & G03.

I know what they mean, I just have no idea how to actually do the math
to figure it out.

I usually use Mastercam to program, but it's pricey and getting old. Any
help would be much appreciated.

I use LibreCAD, an open source 2d cad, when I am writing g-code manually. I use it to find the various end points on a line or curve. If you are not going around in a full circle, you can use R (radius of the curve), instead of I & J (x and y distance from starting point of curve to center of arc).